ABSTRACT

In this paper, four specimens with different thickness of top and seat angle with double web angle connections are experimentally
tested and numerically modeled. The model has been solved by means of Abaqus® finite element package. Moment rotation curves
obtained from the experiments are compared with those obtained from FE models and good agreement is observed. These results
validate this numerical modeling in order to use it in future studies on angle connections.

In conventional analysis and design procedures of steel frames, beam to column connections are assumed to be either perfectly
rigid or ideally pinned. Thus, the true behaviour of joints is disregarded. Moreover, semi-rigid connections have highly nonlinear
behaviour so they are seldom used by designers. On the other hand semi-rigidity introduces economic and structural benefits.
In order to change this trend and to establish a rational design procedure, it is very important to determinate the moment-rotation
characteristics of the semi-rigid connections (1).

One of the typologies of semi-rigid connections is the top and seat angle connection with double web angle. The semi-rigidity
concept reduces the cost and provides structural profits for both steel and composite construction.

The general Eurocode approach is based on a mechanical model that simulates the connection by a series of different components
which are represented by elastic springs. These springs are characterized by a specific stiffness and strength. The appropriate
coupling of these springs in parallel and series provides the global stiffness of the connection. The procedure for calculating
the connection flexural resistance by means of the component methodology can result in a complex task. This complexity is
due to the need of taking into account the interaction between the various bolt rows and the existence of a large number of
components involved in the analysis.

Annex J of Eurocode3 has emphasized the need to account for the influence of the sources of deformation due to the column
(the panel zone components), which can be up to 20 % of the joint deformability. But the main sources of deformation in angle
connections are the angles in bending (up to 70 % of the joint deformability) (2).

Since Eurocode 3 does not consider specifically this type of joint, it is substantial to improve the knowledge about angle
connections in order to make easy its incorporation to European steel design (2). On the other hand, this bolted connection offers several advantages respect to welded joints, especially on the sustainable
construction field (3). In this study, monotonic loading tests are conducted and modeled using European profiles for the analysis of top and seat
angle connections with double web angle.

On the other hand, the Finite Element Method (FEM) has become a powerful tool for investigating the effect of all relevant
parameters related to the connection behavior. Nowadays, with the evolution of computers in solving structural problems, investigation
is usually related to parametric analyses on FE models to investigate the behavior of bolted connections. Considering that
existing tests in literature are related to American profiles and preloaded joints (2), it is very interesting to validate a solid numerical model to deal with future parametric studies on European profiled non-preloaded
connections.

The test set up consist of a pair of beams connected to a central stub column via top and seat angles bolted to the flanges
of the beam and column and web angles bolted to the beam web and column flanges. For practical reasons, the tests have been
developed on reversed configurations and the load has been applied on the column, as shown in Figure 1. Downward movement of the stub column via the actuator resulted in the connection pivoting about a point close to the top
flange angle, placing the bottom flange angle in tension. The tests were carried out in the Structural Analysis Laboratory
of the Higher Polytechnic University College of the University of A Coruña (Spain). The beams were supported on completely
rigid rollers separated 1.5 meters length.

The tests were carried out by means of System 7000 data acquisition system that can be controlled using Vishay Micro-Measurements StrainSmart® software. A 30 tons load cell with sensitivity 2 mV / V was placed under the actuator. Moreover, a couple of inclinometers
were placed on the beams and strain gages were placed in top angles in order to capture the yielding sequence. Finally, the
load was transmitted through an actuator with a load capacity of 30 tons and maximum stroke of 220 mm.

The moment-rotation response has been computed by using the force-displacement data obtained from the tests. The force-displacement
response of the connection is converted to the moment-rotation response using simple relations:

Where M is the moment, ϕ is the rotation of the connection, F is the force, λ is the length of the beam, and δ is the tip displacement of the beam.

3D finite element models of the tests have been performed. The Test 1 3D FE model of top and seat angle connection with double
web angles is shown in Figure 3. Symmetry about the plane of the beam web is used so half of the connection is modelled. The model was meshed by means of
C3D8I eight-node brick elements with full integration and incompatible modes and contact between all surfaces was imposed
with a friction coefficient of 0.3, by using the general contact algorithm of Abaqus® (4). The problem was numerically solved as a quasi-static process by using the Abaqus® explicit solver, because of the ease with it solves complex contact problems, as it was prove in recent works (5). The objective is to model the process in the shortest time period in which inertial forces remain insignificant. The energy
balance results prove the quasi-static nature of the solution since kinetic energy remains negligible throughout the process.

Additionally, the washers were modelled as isolated elements, so that appropriate interactions between components may be developed,
as they have been estimated to be relevant. Finally, the model was improved by introducing the actual length of the beam.

The experimental data describing the stress-strain top angle response is taken from coupon test for Test 1 and Test 2, and
translated to true-stress-strain cuatrilineal relations to be used in the Abaqus® FE models, as it can be observed in Figure 4. For Test 3 and Test 4 coupon tests were not available, so S275 steel nominal values were used. The beam, column and web
angle materials have been introduced with its S275 steel nominal values. The bolts were modelled as elastic components in
order to avoid convergence problems (6).

The load was simulated by an imposed displacement on the column. To achieve the “snug tight” condition, little pretension
has been applied to the bolts by means of a thermal load applied to the bolt shank. The thermal decrease is calculated by
means of the next equation, which disregards the head bolt deformation:

Where σp is the preloading tension in the bolt, α is the coefficient of thermal expansion, E is the modulus of elasticity and εsh is the bolt shank deformation that can be expressed as:

Where Aa is the annulus area (the effective contact area between the bolt head and the plates), and Ash is the bolt shank area:

Where dbh and dsh are the bolt head diameter and the bolt shank diameter, respectively.

Considering that the unthreaded part of the bolt is generally larger than the threaded part, the nominal value of the bolt
shank diameter will be introduced in Equations 5 and 6 in accordance with the bolt geometry related to the FE model.

As it is known, two plastic hinges are developed in the tension angle. The first one is located at the toe of the fillet in
the angle attached to the tension flange of the beam. The second one is located in the vicinity of the bolt line, on the leg
of the angle attached to the column. Abaqus® FE package provides the plastic strain (PE) that is used to represent the material’s inelastic deformation. Figure 5 shows Test 2 plastic strain in the top angle, which is the most important component of this connection typology.

Figure 6 shows that the fit obtained for Test 1 is good, matching the initial stiffness of the MR curve and maintaining the yield
tendency, although with a lower ultimate moment associated. On the other hand, the FE model initial stiffness is larger than
the actual value of Test 2 and Test 3, as it can be observed in Figure 7 and Figure 8. Test 4 FE model fits the initial stiffness but not the ultimate moment, which remains below the test value (Figure 9).

As it can be verified (Figure 10), the numerical models manage to reproduce the angle deformation behavior, which is the fundamental source of strain for
this typology of bolted joints. In Figure 11 the final deformed configuration of Test 4 can be observed.

3D FE models of top and seat angle connections with double web angles made up of rolled European profiles have been developed.

In order to ease the experimental lack in literature and to obtain empirical data for comparing with numerical results, four
specimens on non-preloaded European connections have been tested.

The effectiveness of this modelling approach has been proved by comparison with experimental data, so this numerical approximation
could be successfully used in future parametric studies.

The increase in stiffness and resistance, due to angle thickness growth, has shown the possibilities of angle connections
in European steel construction as an alternative to other semi-rigid typologies.